G76

G76 allow you to make simple fillets and also to make radial contours easier than using G02 or G03. I will start by introducing the G76 fillet command in the same way as with the G75 by using the example from the main page and then I will go into some further details.

A simple external contour

Let me give you an example of a very basic contour that can be the outside of a simple part that will be made by turning.

G0 X20 Z5

G1 Z0 F0.1 G42

G1 X40

G1 Z-30

G0 X45

G40

The code above make a super simple corner but the problem with writing in this way is that the corner will become sharp and this will make it easy to get cuts in your fingers when handling the part, I will remedy this by using G76.

If I rewrite the code above using the G76 command instead of the G1 on the appropriate spot the code becomes:

G0 X20 Z5

G1 Z0 F0.1 G42

G76 X40 L0.5

G1 Z-30

G0 X45

G40

When using the G76 I will make a fillet with radial size L0.5 in this case. If I want to make a chamfer instead of a fillet I could use G75 instead.

By changing the L-value I can give the fillet a different size. I can for instance make the code like this:

...G1 Z0 F0.1 G42

G76 X40 L2

G1 Z-30...

And thus the fillet will have a size of 2mm instead of a half as shown above. This can of course be generalised to almost any value on L, but there are some limitations.

Limitations of G76

The limits of the size of G76 follow the same discussion as those for G75, so I will simply refer you here to that page

G76 for angular contours

Assume instead that we have a contour that is not a simple orthogonal corner but rather has an angle. Presume the contour look like this:

G0 X10 Z5

G1 Z0 F0.1 G42

G1 X20

G1 X35 A120

G1 Z-15

G1 X45 Z-20

G1 Z-30

G0 X50

G40

In this case we have two different angled contours, one using A which give me the angle in degrees and the other using X and Z. Which one to use depends on what is given on the drawing that you receive on the part but using trigonometrics you can switch back and forth.

Let me demonstrate how I would use G76 in the coding example above.

G0 X10 Z5

G1 Z0 F0.1 G42

G76 X20 L0.2

G76 X35 A120 L0.2

G1 Z-15

G76 X45 Z-20 L0.2

G1 Z-30

G0 X50

G40

I have chosen the same L-value in all these cases, this is absolutely not necessary for using the G76 command efficiently, you can use almost any L value you please. Note however that using a L-value which is too large could make an unwanted fillet.

I also want to mention that radial compensation on the tool is very important when choosing the value of L. I can get the same result as above without tool compensation but then I will have to write it like this:

G0 X10 Z5

G1 Z0 F0.1

G76 X20 L0.2+r

G76 X35 A120 L0.2+r

G1 Z-15

G76 X45 Z-20 L0.2+r

G1 Z-30

G0 X50

Assuming that the tool has radius r.

Consideri that the tool I am using has a radius of 0.8mm, then the code above becomes.

G0 X10 Z5

G1 Z0 F0.1

G76 X20 L1

G76 X35 A120 L1

G1 Z-15

G76 X45 Z-20 L1

G1 Z-30

G0 X50

Which will give the same result as the codes above.